I'm still trying to get my setup together for dot-matrix engraving before I start breaking end mills due to runout problems. My first customer wants me to push the state of the art as hard as I can manage it... so I am having to ask the advice from the best again!
Consensus so far seems to be that the original Taig spindle is definitely not the one to use with .003 inch, diameter carbide end mills.
I have been told that the minimum runout on the ER-16 is .0004 inch, and that I should allow .0001 for a collet.
I have Googled around and got wind of the WW spindle. Is it superior to the ER-16? Are there any better solutions for spindles or other low-runout rotational devices?
[The ER-16 is more accurate in terms of runout than Taig's standard proprietary collet. It's about the same as the WW spindle, but more economical. However a .003" cutter will not work too well at 10,000 RPM, the maximum speed of the Taig spindle. You would have to feed extremely slowly to avoid breaking it. For something that small, you would be better off replacing the Taig spindle altogether, and putting on something much faster,
30,000 RPM or above. Here's a good one:
Thanks so much for getting back to me. I contacted them... minimum price of elex spindle is $3800. Yoiks! The ER-16 has a TIR of .0004, minimum. But I found out today about Wolfgang Engineering off Ebay, they have a high speed spindle series with a TIR of .0002.
Yes, the vendor of the .003 cutter strongly suggested a feed rate of
1.5 inches per minute. Slow, but a lot faster than hand-work :)
At the same time, I am also investigating the use of 60 degree included angle V engravers having a .001 point and going in far enough to cut a .003 wide hole. Would that be less vulnerable to runout?
More importantly, why are you trying to run it on a Taig?
I'm not saying you won't be successful. However, chipload versus the minimum resolution of your machine becomes exceptionally important. For instance, a
200 step/rev stepper motor driving a 20 TPI leadscrew gives you .00025"/step. This may very well exceed your endmill's maximum chipload. Also, any mechanical play in your machine could easily break the cutter.
----- Original Message ----- From: "The Eternal Squire" Newsgroups: alt.machines.cnc Sent: Friday, June 02, 2006 12:53 PM Subject: Re: ER-16 vs WW spindle for Taig?
[Yeah, I was too cheap to buy the NSK spindle too, much as I lusted after it in my heart. I did get one of Wolfgang's, and while it does go pretty fast and is variable in speed, it's noisy and vibrates a lot. The worst thing about it, though, is the way it holds bits - there's no way you're getting a TIR of .0002 when you're holding the endmill in it with one setscrew, sorry.]
[Did you tell them you were only going to be running at 10k RPM? Did you mention what material you were trying to cut? These things matter...]
[Runout would be the same, but it would be much less vulnerable to breakage, due to the tool geometry. But when I've tried using these I found they seemed to push the metal up on either side of the cut like a plow, rather than removing it cleanly. I had much better results with a ball endmill, run at less than full depth.]
[I'm sure there is...]
Because a 300 dpi image dictates pels of .0033 inches, and the nearest cutting bit to that is .003 inches
Because it is what I got. I had originally set out simply to use it as a general purpose mill for my own R&D, but then I happened across a possible customer who wanted me to try to do this, if achievale would be be nice work if I can get it.
Excellent point. I had calibrated the axes of my machine using EMC2 on Ubuntu-magma real-time Linux kernel controlling Xylotex drive circuitry, and it turns out that I have 32767 step per inch resolution.
I had gotten a call back from NSK since, and an engineer talked with me. Turns out that for my application I am recommended the HTS-1500. It has a TIR of 20 MICROMETERS!!! (That's effectively zero as far as I am concerned).
It is air-powered, requiring 71 psi at 3.5 cfm. The speed, though, is considerably faster than 10,000 rpm, which would give me an improved feed rate. Can that be an automobile shop air compressor?
It is somewhat less expensive, 'just' (har har) $2900. That's about as much leftover startup cash as I have remaining. So far I have spent $2800 for $5200 worth of Taig and CAD software on Ebay, and a little more for some extras like a bandsaw.
However, there is a demo loan program that according to the engineer I might be able to qualify for, so I could save that cash for getting the other things I need to operate a demo spindle on the Taig. Then when I can demonstrate this to my customer's satisfaction and have confirmed orders, I can put the dang thing on my Visa. Or I could use the V-cutter as discussed below, get what orders I can based on what it can do on my existing mill and spindle as Stage One, and put off buying this spindle until Stage Two.
Meaning that Wolfgang's spindle as good, or just as bad, as the ER-16 collet, right?
Yes, and the metal is 10K gold-filled alloy, and that's why the vendor said 1.5 ipm.
And a ball endmill is what would you use to cut 300 dpi images? If so, what specs?
It sounds like a v-cutter is what you want. Are you merely making dots, or are you moving sideways when cutting?
The reason I was asking is that .003" endmills are very (underline and bold "very") uncommon. I'd be fairly surprised if a taig (I have one) could run a .003" endmill correctly.
In that case, you need only be concerned with mechanical play in your mill. I recommend setting up a dial indicator such that you can push and tug on your machine, and see how far it moves. Basically, if you can setup a stationary dial indicator against your mill table, give the table a bit of a push, and see any movement (a .0001" indicator would be appropriate), it is likely that you would be virtually unable to run a .003" endmill correctly.
As an example, I can put a standard box wrench on a Bridgeport mill's head, and with a slight tug, make it move perhaps .001 or .002" at the spindle nose. In terms of a .003" endmill, it's like running a 1/2" cutter and having 1/8" to 3/8" of play at the spindle nose. Obviously this would quickly break the cutter.
This is probably only an issue if you're moving sideways while milling, as opposed to up and down (drilling).
If you talk to a mold maker, he'll tell you the types of issues he has running small endmills (larger than .003" no doubt) in $100k CNC milling machines with high-speed spindles.
Well, it's important that we understand what your application is. I don't meant to be rude, but it sounds like you haven't got a lot of experience as far as this type of machining is concerned. Hopefully those here can guide you in the right direction before you start snapping very expensive cutters and wondering what the hang's going on. Unfortunately you won't be running under ideal conditions and I suspect you won't have enough experience to reason your way out of this problem when things start going wrong.
Side to side would be nice, but even dots would work for some applications.
I'm beginning to understand from the half-dozen people I am presently asking that v-cutter or conical cutter is really the best way to go, as it is far less sensitive to runout.
Probably the acid test of whether I can use a Taig with this size endmill at all. Even with a 20 micron TIR spindle, the 'play' would still kill any advantage that gives me, right?
I am also beginning to see how I might want to back off to using a .005 or .006 endmill.
No insult taken, I have none at all !!! For reasons I cannot go into here, I have to try anyway.
I don't have the luxury of waiting until I am as trained as all you guys. The best I can do is to read, ask, listen, experiment, try, fail, try, fail, try, fail, try, fail.... and then one day succeed.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.